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surface visability in an idw

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Message 1 of 47
slphantom
3901 Views, 46 Replies

surface visability in an idw

did something change in 2013 as far as the way surfaces are displayed in an idw? the surfaces always always had to be "included" in a idw view. now they come in as regular geometry.

Scott
win 11 64 bit
Nvida GeForce RTX 4000
Inventor Pro 2023
Space Explorer
46 REPLIES 46
Message 2 of 47
rhasell
in reply to: slphantom

Frustrating

 

I have the same problem.

(http://forums.autodesk.com/t5/Autodesk-Inventor/Surfaces-visible-in-IDW/m-p/3612316#M447387)

 

 

Reg
2024.2
Please Accept as a solution / Kudos
Message 3 of 47
JDMather
in reply to: slphantom

Drawing of part (*.ipt)

or

drawing of assembly (*.iam)?

 

Attach your files here.


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Message 4 of 47
slphantom
in reply to: JDMather

Here you go

Scott
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Message 5 of 47
slphantom
in reply to: slphantom

I apologize for all the weird construction features of this part it has gone through many configuration changes to get to this shape.

Scott
win 11 64 bit
Nvida GeForce RTX 4000
Inventor Pro 2023
Space Explorer
Message 6 of 47
slphantom
in reply to: slphantom

yeah i am detailing a machine right now and I have used surfaces for things like rolls in vee blocks for dimensioning purposes. I use to have to "include" them in a view and they came in with properties llike if you included a datum. now i have to go through every view and take them out.

Scott
win 11 64 bit
Nvida GeForce RTX 4000
Inventor Pro 2023
Space Explorer
Message 7 of 47
JDMather
in reply to: slphantom


@slphantom wrote:

yeah i am detailing a machine right now and I have used surfaces for things like rolls in vee blocks for dimensioning purposes. I use to have to "include" them in a view and they came in with properties llike if you included a datum. now i have to go through every view and take them out.


What happened to my response?


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Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


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Message 8 of 47
slphantom
in reply to: JDMather

I only saw the post where you asked me to upload the idw and part.

Scott
win 11 64 bit
Nvida GeForce RTX 4000
Inventor Pro 2023
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Message 9 of 47
Shiva_Sundaram
in reply to: slphantom

Hi Scott,

 

In 2013, we introduced design views in parts. Surface visiibility in drawings is now controlled by part design views. We apologize, its definitely a change in behavior.

 

Here's how you can do it.

1. Open your part file

2. Expand the view representation in the browser

3. Create a new view rep (give it some name: say "AllSurfaces")

4. Click on Surface Bodies folder and turn them off

5. Switch to drawings

6. Edit the view and select the viewrep (AllSurfacesOff)

 

The view should update and all surfaces should become invisible.

 

The behavior is just like assembly design views to control visibility of components.

 

Hope that works out.

 

Thanks

-Shiva Sundaram

Inventor Development

 

Message 10 of 47
rhasell
in reply to: Shiva_Sundaram

Thank you Shiva.

 

Reg
2024.2
Please Accept as a solution / Kudos
Message 11 of 47
Shiva_Sundaram
in reply to: rhasell

Hi Reg,

 

No problem. Hope that works out. Sorry I forgot to address you in my post.

 

-Shiva Sundaram

Inventor Development

 

Message 12 of 47
slphantom
in reply to: Shiva_Sundaram

so now i have an existing assembly idw and i added this part i downloaded from a vendor site and it does not show up on the idw views. how do i fix this?

Scott
win 11 64 bit
Nvida GeForce RTX 4000
Inventor Pro 2023
Space Explorer
Message 13 of 47
Shiva_Sundaram
in reply to: slphantom

Hi Scott,

 

Does it appear if you create a new view? If so, then you may want to check to see if the drawing view (which doesnt show the part) has Associative DV = ON (view dialog has a checkbox). If its unchecked, you click on that to make the view associative, the part should become visible by default whenever any part is added to the assembly.

 

OR you can re-apply design view to an existing drawing and right click context menu.

OR you can select the part from the browser and turn visibility ON (if its off)

 

If new drawing views also do not  show that, then it might be a problem with the part and I would be happy to take a look at if you want to email it to me - sundarsATautodeskDOTcom

 

Thanks

-Shiva Sundaram

Inventor Development

Message 14 of 47
slphantom
in reply to: Shiva_Sundaram

it shows it as on in my idw browser and if i create a new view of the same it shows up. i got it to show up in other views so just that top level assy idw. i can work around it.

thanks

Scott
win 11 64 bit
Nvida GeForce RTX 4000
Inventor Pro 2023
Space Explorer
Message 15 of 47
rhasell
in reply to: slphantom

Hi

 

Back again. How do you set the view rep for Assemblies?

 

The parts have the surface switched off, the surfaces are not visible in the assemblies, you can't acces the suface in the assembly tree either, but yet they all come through in the IDW?

 

 

SURFACE VIZ.JPG

Reg
2024.2
Please Accept as a solution / Kudos
Message 16 of 47

Hi Reg,

 

Did you try creating a drawing view with the View Representation CHECKED. The view create/edit dialog should contain a checkbox and if you click on it, it will use the view rep from the assembly document. Make sure that when you create or edit the drawing view, you select the view rep (in the list) which corresponds to the one which has surfaces off.

 

I know it's a little confusing and change in behavior....

 

Thanks and hope that helps....

-Shiva Sundaram

Inventor Development

 

Message 17 of 47
cellt2
in reply to: Shiva_Sundaram

I don't think this is just "confusing" or a "change in behaviour".  This is a major addition to the work load and I cannot understand what has possessed AD to hobble its users this way.

Message 18 of 47
rhasell
in reply to: Shiva_Sundaram

Thanks Shiva

 

I will try the different workflow.

 

I gave the workflow a quick test, and guess what, it all worked 100%

 

The Assiciative check box was not ticked, on that particular drawing, I will keep you updated if find anything strange.

 

Applying "All surfaces" view rep is still quite painfull.

 

tx

 

Reg
2024.2
Please Accept as a solution / Kudos
Message 19 of 47
chrisreynolds
in reply to: cellt2

We are having the same problem, we make mould tools & use the Sculpt command a lot, we copy the part to be made into various details & cut the surfaces away, every file in Inventor now has a surface visible in it, we have to turn them off in the part ipt file, this is not carried over into the assembly as it did previously, so they all have to be turned off individually in the iam file, then all the drawing views need the same doing to them regarding surface visibility.

 

This is making the process a lot longer & a lot more difficult to follow, can it be put back to how it used to be? we only use it as construction as I imagine a lot of other users do.

Message 20 of 47

Hi Chris,

 

Point taken. I do agree that this is painful. We are looking to see if drawings can ignore surface visbilities and switch back to the old behavior - no ETA yet though :(. For the moment, like i said in an earlier post, the workaround is to use design views in the part to control surface visibility and turn them off prior to using them.

 

-Shiva Sundaram

Inventor Development.

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